9

ANSYS/LS-DYNA 5.7

New Features Demonstration

This workshop demonstrates several new features in ANSYS/LS-DYNA 5.7. An initial velocity (EDVEL) is applied to a rubber ball (TB,MOONEY) which impacts a rigid body plate - the inertia properties, of which, are user-defined (EDIPART). The ball bounces off of the plate, which pivots about its center of gravity (located above the meshed portion). The motion of the plate is restricted by springs and dampers (TB,DISCRETE), which cause the plate to swing back after the kinetic energy from the ball is converted into internal energy in the springs. The cube becomes a projectile on impact with the plate. The analysis is then stopped. On restarting the analysis (EDSTART,2), the rubber ball is converted into a rigid body (EDRD,D2R) to reduce the CPU time. A termination criteria (EDTERM) is set to stop the analysis for the second time when the ball reaches a specified location. In the subsequent second small restart, the rigid ball is converted back into a deformable body (EDRD,R2D) so that stress data can be saved.

Brief Instructions

  1. Enter ANSYS in the directory specified by the instructor
  2. Read in the first input file, dyna57a.inp (/INPUT)
  3. Define the Mooney-Rivlin material properties (TB,MOONEY)
  4. Define the initial velocity conditions for the ball (EDVEL)
  5. Read in the second input file, dyna57b.inp (/INPUT)
  6. Create the part list (EDPART,CREATE)
  7. Define inertia properties for the rigid block (EDIPART)
  8. Set up the contact between the ball and the block (EDCGEN)
  9. Define the material properties for the springs (TB,DISCRETE)
  10. Read in the third input file, dyna57c.inp (/INPUT)
  11. Set up the first small restart analysis (EDSTART,2)
  12. Specify the termination time (TIME)
  13. Switch the rubber ball to a rigid body (EDRD,D2R)
  14. Set the termination criteria (EDTERM)
  15. SOLVE the first restart and review the results in POST1
  16. Set up the second small restart analysis (EDSTART,2)
  17. Extend the termination time (TIME)
  18. Switch the rigid ball back into a deformable body (EDRD,R2D)
  19. Remove the termination criteria (EDTERM)
  20. SOLVE the second restart and review the results in POST1

Detailed Instructions

  1. Enter ANSYS/Multiphysics/LS-DYNA in the specified directory.
  1. Create the ball geometry with the input file dyna57a.inp

Utility Menu > File > Read input from … > dyna57a.inp > OK

  1. Create the stress-strain curve that represents the rubber data. The stress and strain arrays were previously defined and filled (see dyna57a.inp).

Preprocessor > Material Props > Curve Options …


OK

  1. Define the material properties for the rubber ball:

Preprocessor > Material Props > Define MAT Model … > ADD > 1 >

Non-Lin Elastic > Mooney-Rivlin > OK

Test Data Calcs

OK

  1. Enter the data shown below. Setting the specimen dimensions to “1.0” informs LS-DYNA that the specified load curve contains engineering stress versus engineering strain data (instead of load versus deflection data). Both of these options force LS-DYNA to calculate the Mooney-Rivlin coefficients. Alternately, the two-term form of the coefficients could have been entered directly...

OK

Close

  1. Use EDVEL to enter the initial velocity data for the ball:

Preprocessor > LS-DYNA Options > Initial Velocity > w/Axial Rotate …


OK

  1. Create the pivoting rigid block with the input file dyna57b.inp

Utility Menu > File > Read Input from … > dyna57b.inp > OK

  1. The Part list is needed to assign inertia properties:

Preprocessor > LS-DYNA Options > Parts Options > Create parts > OK

File

Close

  1. Specify the inertia properties for the rigid body plate as shown below. The portion meshed represents only the bottom section of the plate. Since rigid bodies rotate about their mass centers, placing the CG above the portion meshed will allow the rigid body plate (Part 2) to pivot when impacted by the rubber ball (Part 1). The mass center vector (p2cg) and the inertia tensor (p2inert) have already been defined, so the select options will be used.

Preprocessor > LS-DYNA Options > Inertia Options > Define Inertia


OK


OK


OK

  1. Verify that the correct part inertia properties were specified:


File Close

  1. Define Nodes-to-Surface (NTS) contact between the ball and the rigid plate.

Preprocessor > LS-DYNA Options > Contact > Define Contact



OK

OK

  1. Specify the spring stiffness for a linear elastic spring (TB,DISCRETE):

Preprocessor > Material Props > Define MAT Model … > ADD > 3 >

Discrete > Linear Elas Sprn > OK


OK

Close

  1. Create the rest of the ANSYS/LS-DYNA model with the input file dyna57c.inp. This input creates the spring and damper elements that restrict the motion of the pivoting rigid plate and the mass elements attached to the springs. It also creates an elastic cube (initially at rest) that becomes a projectile when the spring elements pull the plate back, thereby striking the cube. A fixed rigid plate is also created to intercept the rubber ball after the latter bounces off of the pivoting plate. The associated contact definitions are also defined.

Utility Menu > File > Read Input from … > dyna57c.inp > OK

  1. Due to the limited amount of time for the workshop, the input file also sets the analysis options, including the termination time. The output frequency of the results files is set with the new DT (delta time) option on the EDRST and EDHTIME commands. Likewise, the frequency of writing the d3dump restart files is controlled by the new EDDUMP command. The input also starts the first solution. Please wait until it finishes before continuing with the exercise. Consult the input file dyna57c.inp for more information.

  1. Request the first small restart analysis (EDSTART,2).

Solution > Analysis Options > Restart Option


(Note: You may need to first reset your preferences to LS-DYNA)

OK

  1. Extend the termination time (TIME) to 0.020 seconds.


Solution > Time Controls > Solution Time

OK

  1. Convert the rubber ball (Part 1) into a rigid body (EDRD,D2R) to reduce the required CPU time as it travels untouched through the air. It is only possible to switch parts (D2R or R2D) in a restart if part switching was first activated in the original analysis. The input file dyna57c.inp accomplished this by issuing the command EDRD,D2R (with no further arguments) in the first analysis.

Solution > Rigid-Deformable > Switch


OK

  1. Set the analysis termination criteria (EDTERM) to be the global Z position of the node at the center of the ball, nballctr. By stopping the analysis when the node reaches a specified location, the rubber ball can be converted back into a deformable body prior to impact with the fixed rigid plate. Other termination criteria exist, as well, including those for part displacements and for detection of contact.

Solution > Analysis Options > Criteria to Stop > On a Node


OK

  1. Save the database and initiate the first small restart analysis.

ANSYS Toolbar > SAVE_DB

Solution > Solve > OK

  1. Review the results in POST1

General Postproc > -Read Results- Last Set >

Plot Results > -Contour Plot- Nodal Solu … >

Stress > von Mises SEQV > OK

  1. Request the second small restart analysis (EDSTART,2). Be sure to pick up where the last analysis finished (i.e., use the 2nd restart file, d3dump02).


Solution > Analysis Options > Restart Option

(Note: You may need to first reset your preferences to LS-DYNA)

OK

  1. Extend the termination time (TIME) to 0.025 seconds. Note that the previous restart stopped at TIME=0.0167 seconds, due to the EDTERM criteria.

Solution > Time Controls > Solution Time


OK

  1. Convert the rubber ball (Part 1) back into a deformable body (EDRD,R2D) now that impact (with the fixed plate) is about to occur.

Solution > Rigid-Deformable > Switch


OK

  1. Remove the analysis termination criteria (EDTERM) defined in the first restart analysis to prevent immediate termination of the second restart analysis.

Solution > Analysis Options > Criteria to Stop > On a Node


OK

  1. Save the database and initiate the second small restart analysis.

ANSYS Toolbar > SAVE_DB

Solution > Solve > OK

  1. Review the results in POST1

General Postproc > -Read Results- Last Set

Utility Menu > PlotCtrls > Animate > Over Results

Load Step Range - Range: 1 (Min) to 3 (Max) -

Increment: 5 - Auto contour scaling: Off -

Animation time delay: 0.5 - Stress - SEQV - OK

  1. Exit ANSYS …

ANSYS Toolbar > QUIT > Exit without Saving > OK

ANSYS 5.7 New Features Workshop Supplement9-1